[ Log In ]
[ Register ]
From Sketchup to CNC Fabrication and Built Assembly
In this tutorial, I show you how to draw a complex assembly in SketchUp, take that drawing and build upon it with machining operations (tool paths) in CAM, cut out the parts on the greenBull CNC Machine, and build the assembly completely.

The CAM program used to apply the machining operations (drill, profile, pocket, etc.) is CAMBAM; however SketchUp's output dxf can be used with pretty much any CAM program out there. The assembly being designed and fabricated is a shelf with wheels that is used for the blackTooth Laser Cutter and Engraver.

In this final video, the fabrication process (cnc machining) is shown and explained. The parts are not just cut out on the CNC machine, but also undergo a process of manual drills and cleanup.

The CNC machine is setup with a new sheet loaded onto the spoilboard (the board that gets the hurt from many CNC jobs and is fastened to the table of the CNC). The CNC machine is homed by manually jogging to the spindle to the origin we determined in the CAM process. The file from the CAM process is loaded into the computer that is connected to the CNC machine and the fabrication is started.

The build of the assembly is also shown to round out the entire process.

In this video, the assembly is being designed and drawing in SketchUp. Since this is not a tutorial on using SketchUp, the drawing and designing portion of the video is sped up, but many of the design considerations can be seen. The point of this video is taking the 3 dimensional assembly and preparing it for use in a CAM program.

First, the parts are all laid out on sheets just like they will be cut out on the CNC machine. The parts are arranged in a way that the sheets are utilized as much as possible and the remainder is reduced for reuse. The parts are spaced away from each other so that the end mill (bit/cutter) can fit between the pieces and that there can be a roughing pass and finishing pass. Additionally, the spacing of the parts by just a little more than the diameter of the bit can reduce the wear of the bit since during half of the passes, the end mill is only cutting very little material, since the material was already cut from the part next to it. While the parts are arranged, the parts are oriented so that the counter bores and pockets are facing up. This will help in the CAM side of things.

Second, all of the parts are exploded so we can remove the faces and geometry not needed in the CAM process. After the parts are exploded, any z geometry and back lines and polygons are removed. These are not needed as it will just double up on the geometry that we need. The faces are also removed to eliminated for the same reason. You might be wondering, why the faces are removed but the line and polygon geometry (on the top face) is kept. When faces are transferred to the CAM program, they contain the same geometry, but certain geometry, like circles, are just polygons made up of small lines. The actual geometry that we keep remains as circles, arcs, lines and polygons as we would expect. However, there is a peculiarity, that I will mention during the CAM process. The pocket and counter-bore geometry should be kept so that we can use that in the CAM process to determine the depth that we need to create those machining operations.

Finally, the geometry that remains is saved as a .dxf file. This is easy if you have the pro version of SketchUp. If not, you will need to pick up the free dxf or stl export utility for SketchUp, but be warned, the circles will be transferred as polygons made up of many lines and all of the circles will need to be re-drawing in CAM.

If you don't have the pro version of SketchUp, here is a small tutorial on how to convert the SketchUp geometry using the free plug-in mentioned previously.

The file that was exported from SketchUp is opened in CAMBAM. The first obvious visual problem is the dots/circles on the left of the origin. This is derived from the circles having a normal of -1 which is opposite to the normal that these circles need. Fortunately, there is a simple solution. Since CAMBAM places these circles having normals of -1 mirrored about the y-axis of the origin, the circles can be mirrored about the origin using the mirror command from the CAD Extras plug-in.

In the example shown, all of the arranged parts are shown in an orientation that does not work very well, but a quick rotation of these arranged parts puts them in a good orientation to start the machining operations. It's good to check the geometry to determine all of the geometry was transferred and transferred correctly.

I show each part and the primitive geometry given machining operations, profiles for polygons, pocket for pockets, and drills for medium to small circles (I generally use an inside profile for large holes so I can use holding tabs to hold the scrap so that these don't pop-up and jam the machine during the fabrication process).

The final part of the CAM process is managing the holding tabs. Each part should contain holding tabs unless a vacuum table is being used. The holding tabs are strategically places so that the parts will remain solid while the machine is in the cutting and finishing process. The tabs are generally used to 'stick' parts together and hold them in place, but also to hold the scrap around the corners of the parts that may be left over. If holding tabs are not placed above each other, then the cutting process will remove the tabs when the parts are cut.